Chapter 7

FLACS-CFD Best practice

This chapter presents examples and best practice guidelines for FLACS-CFD. The examples also include simulations that require special variants of FLACS-CFD, such as FLACS-Fire.

There are several ways to create, for example, a door opening in a wall or vessel. This section discuss two different approaches to this problem.

In summary, the main rule is that the grid should fit the vent opening. Then both methods are equivalent. If you have to choose (the vent opening and grid resolution simply do not fit, no matter what you do), then use the approach that will give you a vent opening that is as close as possible to the real one while reducing the number of partially porous cells/faces to a minimum. It is recommended to carry out a small sensitivity study to estimate the effect of the geometry representation.

Make the wall with three boxes.

The advantage of this method is that there is no left difference operation which might be difficult to create and maintain. The disadvantage is that the opening area may be adjusted by the porosity calculator to match the grid. If the boxes are expanded, then the opening area, which is critical for explosion pressures, may be wrong. Therefore, if this method shall be used, then it is important to make sure that the grid matches the door properly. Alternatively, a pressure relief panel can be used, but again, the opening area must be prescribed properly relative to the grid.

Define the wall and door as two flat boxes, and subtract the door from the wall with the help of a left difference operation.

This method will give the exact correct vent area (or rather: the correct blockage ratios based on the opening area), irrespective of the grid resolution, since the area of the opening does not get changed due to adjustment to grid lines. There are examples of simulations where high turbulence has been seen outside a vent opening defined in this way. For situations with circular vent openings/panels this method can be used (combined with a wall at least two grid cells thick) to ensure proper representation of the vent opening.

With the second method, you can get sub-grid contributions around the vent opening if it does not hit the grid properly, and subsequently too high turbulence generation and therefore too high pressures.

When a left difference is used to define (part of) a flow domain and the boundary of the “hole” made by the left difference object is exactly on the domain boundary, then special care has to be taken to make sure the domain boundary is closed. Otherwise, depending on the boundary condition, flow can occur across a boundary that was meant to be closed.

An example of this might be defining the lower domain boundary exactly on the floor of a cellar which has been defined by a left difference box in the ground. An extra zero-thickness box can be used to block the flow at the domain boundary coinciding with the border of the left difference operation.

In FLACS v10.8 two significant improvements have been made to left difference operations:

The first point means that by using the Mark command a left difference can be created in the middle of the primitive list. Prior to this improvement left difference operations could only be created at the end of the primitive list between the last two nodes. An example of this feature can be seen in figure below.

Figure 7.1: Using the Mark command to create left difference

In this figure the Mark command have been used to mark a cylinder in the middle of the primitive list. The marked cylinder will be used as the solid part when adding a left difference. In addition to marking the cylinder the first box in the primitive list have been selected. The selected box will be used as the minus part when adding a left difference. Adding a left difference at this point will subtract the box from the cylinder and add the left difference operation to the end of the primitive list.

Left difference operations can consist of all node types, including named unions and left differences. In the figure below a nested left difference operation is shown.

Figure 7.2: Nested left difference operation

Nesting left difference operations means that it is possible to create geometric objects that it was impossible to model in previous versions of FLACS.

In FLACS-CFD, the scenario variable GROUND _ ROUGHNESS defines the aerodynamic roughness that characterizes the terrain surface throughout the simulation domain. Aerodynamic roughness has a strong effect on velocity and turbulence close to the terrain level. This means that, for releases that occur or develop close to the ground, the resulting extension of the flammable cloud is very sensitive to the ground roughness. flacscfd adopts a modified form of the wall functions at the terrain surface to account for ground roughness (see Rough wall boundary). To activate the ground-roughness-based wall functions at the terrain surface, a terrain file must be created. This can be done in CASD either by importing a DEM file or by converting a geometric object to terrain (see section Convert). This latter option can be used to define a flat terrain at the bottom of the simulation domain from a box created in CASD's geometry editor.

In FLACS-CFD, the computational mesh is composed of cubic or rectangular grid cells (or control volumes) defined by vertical and horizontal grid lines, i.e., a single-block rectilinear grid. The mesh spacing can be varied in any of the Cartesian directions. However, it is not currently possible to fit the mesh to curved or inclined walls or objects and so these are modelled using stepped walls and/or sub-grid models.

Simulations calculated at finer grid resolutions, or over larger domains, take longer to run, see figure below, and so the resolution should be chosen such that a sufficiently accurate prediction is achieved within an acceptable time frame. It is recommended that simulations that are expected to run for days are first calculated for a coarser grid to check the setup and scenario definition (even if the configuration of the

coarser grid does not meet the recommendations outlined in the grid recommendations table).

^^ -8 oios」ll nd9 / (S」H nd。)

Figure 7.3: How the computational cost increases with grid resolution for gas explosion simulations from some experiment campaigns in our validation database. Lines are fitted to data from simulations of individual experiments (colours show experiments from the same campaign). All the plotted simulations were calculated using the same Gexcon HPC.

FLACS-CFD requires the simulation domain to extend beyond the region(s) of interest to avoid boundary effects impacting on results. For this reason, the grid generally comprises one or more high resolution domains, referred to as core domains, and a so-called stretched domain, which extends from the core domain boundaries to the total domain boundary. Cells in the stretched domain may increase in size as the distance from the core domain edge increases and the total domain boundary is approached.

In addition to the core and stretched domains, some scenarios require an area of local grid refinement, where very high resolution is required to resolve a specific feature, and these areas are referred to as refinement regions.

For pool scenarios, the horizontal and vertical dimensions of the core domain are considered separately and an extra domain, the vertical pool region, is required between the bottom of the pool and the base of the core domain to ensure sufficient resolution for the evaporation calculations. Figures to illustrate the different parts of the grid needed for pool scenarios are provided in Grid domains for pool scenarios.

Large differences in size for neighbouring cells can cause problems for FLACS-CFD, so it is recommended that these are avoided and the Smooth tool in CASD can be helpful for creating a smooth transition between

sizes, see the figure below for an example of this.

Figure 7.4: Smoothing the grid around a leak.

The edges of large objects (objects that occupy more than 1.5 grid cells, e.g., walls and decks) should be aligned with the grid, and ideally positioned so that their edges fall on grid lines. Grid planes for an existing grid can be adjusted using the Add , Position and Smooth options in the Grid information menu in CASD.

If an imported geometry is not aligned with the XY grid axes, the Auto-align geometry can be used to automatically align it.

Porosity is calculated for each grid cell and if the edges of large objects are not positioned on grid lines then undesirable artifacts may result, such as “leaking corners” or enlarged/shrunken vent areas. If a large surface does not sit on a grid plane, then secondary objects may create porosity profiles that lead to inappropriately increased turbulence at the deck surface, e.g., beams may be considered in the calculations to be on top of the deck instead of below it. It is not necessary for small objects to be aligned with the grid unless they are the dominant structures in a scenario, e.g., in a geometry with only a few objects.

For some complex scenarios, it may not be possible to align all large objects with the grid and still comply with the grid recommendations below. In such cases, it is recommended that large objects which are closest to the ignition are aligned, and other objects are aligned as far as is possible. The extent of any misalignment of large objects with the grid should be considered when interpreting simulation results.

The inner diameter of angles and bends should be increased slightly when modelling pipes using a cylinder minus primitives. The solid wall around “minus primitive holes” must have a thickness of at least one full grid cell to ensure no leakage through the wall (two cells may be better when a cylinder is “subtracted” from another cylinder). A check to confirm that the predicted flow behaviour is as expected is recommended.

When the geometry is projected onto the grid, it is important to ensure that there are no partial openings

where two geometry objects (e.g., pipes or vessels) are joined. This should be checked by calculating and verifying the porosities after creating the grid, see the Porosities menu in CASD.

For more information on defining geometry and positioning it appropriately for the grid, see Representing geometry in the Geometry chapter.

The recommendations in the table below describe the optimum configuration of the grid according to the scenario characteristics. These are based on validation against experiment results and on an analysis of the calculations in FLACS-CFD. For many scenarios, it is not possible to meet all the recommendations, for example orientating the grid so that all leak directions are aligned with grid axes. In such cases, the recommendations should be followed as closely as possible and a grid sensitivity study may be helpful.

Multiple recommendations in the table apply to any individual scenario and the first column can be used to determine whether each specific recommendation is applicable. Some recommendations are based on information that may not be readily available, such as the initial high pressure region for a blast. The notes below the table provide references to sections of this manual where methods for estimating these are provided.

Once configured, some aspects of the grid configuration can be checked using the grid checking option in CASD.

Grid sensitivity studies are recommended for dispersion simulations (see below). For explosions, it may be beneficial to perform grid sensitivity simulations if the guidelines result in resolutions that are too fine for practical simulation (e.g., because of memory resources or because cells smaller than 1 cm are not recommended). Our validation for explosions is based on resolving the gas cloud with 15 cells, and simulations generally converge to the experimental results in this region (although they may diverge at finer resolutions for some scenarios). Numerically, the code does not fully converge with increasing resolution, primarily due to interactions between the structured cartesian grid, the geometry, and porosity. Our validation data are used to tune the models in FLACS-CFD so as to achieve our most accurate results when the clouds is resolved with 15 cells. This resolution allows simulations to be calculated within engineering timescales, while being sufficiently refined that small changes in the resolution generally do not result in large changes to the simulated data (for example, moving from 15 cells to 16 or 17 cells). Grid resolutions in the region of that which resolves the cloud with 15 cells therefore constitute a region of local convergence in most cases. In some cases, sensitivity could be looked at over the range of about 14 to 17 cells to determine if more extreme grid sensitivity is seen for a particular scenario.

Gas dispersion is affected by several parameters, including air and gas densities and velocities, and the size, position and complexity of any geometry in the scene. It is important that the grid resolution is sufficient to resolve all expected gradients. Sensitivity to the grid resolution varies between scenarios and so a sensitivity study is generally recommended. However, this is not always practical and several validation studies have

therefore been carried out to determine the recommendations in the table.

Different grids are appropriate for dispersion and explosion simulations and so results from a dispersion simulation should be dumped and regridded before being used to simulate an explosion (see Combined dispersion and explosion simulations).

They do not check that the grid is as coarse as possible (i.e., a coarser grid may also meet the recommendations).

When this applies

Recommendation

Notes

ALWAYS

Grid does not extend unnecessarily below an impermeable ground surface (and ground covers whole of the horizontal domain).

ALWAYS

Cell size at all ROI(s)+ < 5 m.

This ensures that all values are meaningful (further recommendations below will result in a smaller value for most scenarios).

This may need to be increased to avoid an impractically high number of grid cells for dispersion and fire simulations that cover a very large domain. Cell sizes of up 20 m have been used successfully for simulations with ROI(s)+ that are 500 m from the source.

ALWAYS

Stretch factor** < 1.2.

Stretch factors++ beyond 1.2 have not been widely tested and are not generally required. However, it may be necessary to use a slightly higher stretch factor++ for a dispersion scenario which otherwise requires an impractical number of grid cells, or where the grid has been adjusted to fit a wall. It is not anticipated that results will be adversely affected provided the factor remains below 1.4, but this has not been widely tested.

ALWAYS

At least 3 cells between the total domain boundary and any ROI+.

This makes it less likely that values are impacted by any unphysical boundary effects.

ALWAYS

Monitor points should not be in the same grid cell as a solid wall (unless the wall is thicker than a single grid cell or forms the simulation boundary, e.g., the ground).

The wall may snap to a cell wall that means the MP is on the other side of it from what was intended.

Note that MPs may be placed in a cell that is bounded by a wall (or panel) with thickness = 0 if the wall (or panel) is positioned on a grid plane.

ALWAYS

Monitor points should be in unblocked cells.

Ideally, monitor points should be in porosity=l cells. If this is not possible, then we should try to maximise the porosity of the MP cell. If neighbouring cells have higher porosity, then we should move the MP so that it is just inside a neighbouring cell. If neighbouring cells also have low porosity, then a finer grid resolution may be needed to capture any space around the MP.

Explosion, blast and fire

Cell size in all domains > 1 cm.

Cell sizes smaller than this have not been widely tested are there is a possibility that the subgrid models may fail, in particular the sub-grid model for premixed combustion (explosions) may severely overpredict burning velocities for very fine resolutions.

Where a scenario is particularly fine-scaled (or where grid refinement is needed around a very small feature, e.g., a small point leak), then cells may be smaller than this, however it is recommended that results are checked carefully and if any artifacts are present that indicate model breakdown, then a coarser resolution should be used. Finer resolutions have been tested for some fire scenarios and accuracy has not been adversely impacted.

Blast

Monitor points should not be cells with porosity = 0.5

FLACS-Blast treats porosities as binary, so porosity=0.5 cells are ambiguous.

Any scenario with an ignition/explosive location

Ignition should not be on a grid line and should be in an unblocked cell.

See note above about recommendation for MPs in unblocked cells.

For blast scenarios, the explosive location may be in a partially blocked cell but an initial simulation should be used to check that the high temperature and pressure region do not partially penetrate the wall.

Any scenario with an ignition

Ignition should not be in the same grid cell as a solid wall.

See note above about about the same recommendation for MPs.

Explosion

Aspect ratio** for cells in core domain* < 2.

The longest cell side should be no more than twice the length of the shortest cell side.

Blast

Aspect ratio** for cell sides in the horizontal plane in the core domain* =

If Z is vertical, then the lengths of the X and sides of cells in the core domain should be equal. Cells may be elongated in the Z-direction by up to a factor of 2 if the wave propagation in this direction is not of interest (otherwise cells should have an equal length in X, Y and Z).

Gas explosion with vents+++

Minimum distance from vents+++ to core domain* boundary:

  • •    7 cells in vent-opening direction

  • •    5 cells in all other directions.

Dust explosion with vents+++

Gas explosion when an external explosion is likely

Minimum distance from vents+++ to core domain* boundary:

  • •    3 x vessel length in vent-opening direction

  • •    7 cells in all other directions

Recommended for all dust explosions to ensure that any external explosion is sufficiently resolved.

For a gas explosion, an initial coarse-resolution simulation may help to determine whether an external explosion is likely. The possibility of external explosion should always be considered when the fuel mix includes hydrogen.

+ ROI region of interest. This is any monitoring point or region where values calculated in FLACS-CFD are of interest.

++ The stretch factor is the length of a cell in one direction divided by the length of the neighbouring cell in the same direction.

+++ Vents are openings that may or may not be covered by panels (so panels are treated as vents).

The core domain(s) are region(s) of the grid where higher resolution is required (e.g., close to a leak, where there is a flame, the gas cloud for an explosion,..). Note that some further refinement is required around point leaks and immediately above an evaporating pool surface. See Grid domains in the manual for more information on naming parts of the grid.

See the "Jet flame shape,f section in the Technical reference chapter for a method to estimate the jet flame shape plus lift-off (implemented in the automatic grid refinement in CASD). This ideal flame shape does not account for congestion or impingement, so it is recommended to use an initial coarse-resolution simulation to estimate the flame dimensions for congested scenarios.

See the MMaximum pool area and flame shape for pool scenarios" section in the Technical reference chapter for a method to estimate pool flame shape and the maximum area for a spreading pool. This ideal flame shape does not account for congestion or impingement, so it is recommended to use an initial coarse-resolution simulation to estimate the flame dimensions for congested scenarios.

The jet utility can be used to estimate the expanded leak area (implemented in the leak wizard in CASD and described in the Release source modelling section of the Utility programs chapter) or, alternatively, follow the section * Steps when the jet utility program is not employed, in the manual.

The Technical Reference chapter provides a method to estimate the high pressure region where shock waves greater than 1 barg are experienced following a blast.

This estimate does not account for reflections from surfaces (other than the ground), which may increase the blast volume. It may be necessary to extend the core domain beyond this minimum extent for these cases.

Alternatively, an initial coarse-resolution simulation can be used to estimate the distance travelled by the wave. The Technical Reference chapter provides a method to estimate the initial high pressure region.

Attention:

Pool and dispersion scenarios with non-zero windspeed require a secondary core domain with the same extent and resolution as the primary core domain described in the table. The secondary core domain should be located with its centre offset from the primary core domain centre by a distance equal to the pool radius, in the wind direction. For an area leak, the offset distance should be the distance from the leak centre to the leak edge in the wind direction. This is not needed for jet fire scenarios since the flame shape estimate that is used to set the core domain accounts for windspeed.

Some of the recommendations in the table should be adjusted slightly for the special case of modelled-entrainment leaks, as described in the Entrainment functionality section.

There are at least three different ways to perform a combined dispersion and explosion simulation in FLACS-CFD:

dispersion simulation. Also with this approach it is not possible to use the WIND condition because it enforces a fixed velocity, which is not applicable in the explosion (cf. Wind boundary condition).

Create a directory for the example and copy the files from

/usr/local/Gexcon/FLACS-CFD_22.2/doc/examples/ex04_dispersion/*00001*

as described in section Creating the work directory. Start the FLACS-CFD RunManager.

In the RunManager, use Add Directory to find the directory that contains the geometry files. Use RunManager T Tools T CASD (or click the FLACS-CFD pre-processor icon). Open the file 200001.caj (and ignore any error messages that appear). The geometry is a representation of a full-scale process module. The dimensions are28 m 12m 8 m.

Measure FMOLE and UVW at monitor points by selecting all monitor points, right click and select 'Edit'.

Measure FMOLE, ER and VVEC for 3D-output (see the Single field 3D output section). Remember to hold the CTRL key while selecting multiple variables for output.

Figure 7.5: Specification of monitor points

Figure 7.6: Specification of the WIND boundary condition

For the logarithmic wind profile, set the Reference height to 10, and Ground roughness to 0.01. The Pasquill class must be F. Leave the other parameters unchanged.

Figure 7.7: Specification of initial conditions.

Double-click on Outlet. Use a mass release rate of 4 kg/s through a 0.02 m2 leak area. Set the initial turbulence for the leak: relative turbulence intensity = 0.2, turbulence length scale = 10% of leak diameter = 0.014, Temperature = 20 degC, leave the direction cosines as (0, 0, 0).

1.33 m                           0.1581 m                          1.33 m

Figure 7.8: Sketch of the grid refinement.

Creating the refinement region

The leak is at Y = 5.05 m and grid lines should be created (3/2) &times 0.1581 = 0.237 m from this in both directions, at 4.813 and 5.287 m. In the Grid menu in CASD, set the grid direction to Y and use Add to add these two grid lines. Select these two grid lines using CTRL and arrow keys (a message in the yellow box below the CASD geometry window shows which grid lines are selected).

Smoothing from the refinement region

Select Region from the Grid menu and enter 3 to create three grid cells of size 0.1581 m. Now smooth the grid between the two significantly different cell sizes. Select grid lines between -1.333 m and 4.975 m so that grid cells a distance of 4-5 cells from the refined cells, and one refined grid cell, are selected. This defines the region over which the grid will be smoothed (the size of the cell at each end of the smoothing region will remain unchanged by the smoothing, see Smooth). The grid spacing should not change by more than 20% from one grid cell to the next (see grid recommendations); if this cannot be achieved within the

selected smoothing region, then the region must be extended further from the refinement region, i.e., to Y &lt -1.333 m. The module edges must remain positioned on grid planes, so grid lines are required at Y = 0 and 12 m. If the smoothing has caused these lines to be moved, then grid planes in the smoothed region should be manually adjusted using Move from the Grid menu. Repeat these smoothing steps to smooth between the maximum extent of the refinement region and the ambient grid in the positive Y direction. All dimensions

The steps described above for refinement in the Y-direction should also be followed to refine the grid in the X- and Z-directions. No smoothing is required between the refinement region and the ambient grid in the negative Z-direction because the refinement region in this direction is bounded by the ground. Smoothing should be carried out following the steps described above in the X-direction, and in the positive Z-direction. Following all refinement and smoothing, Information can be selected from the Grid menu to check that the maximum size difference between neighbouring cells does not exceed 20%.

Figure 7.9: Grid in Y-direction

The last step before starting the simulation is to make a cc-file. In the FLACS-CFD RunManager, click on the dispersion job, click parameters, and edit cc-file and type the following (use capital letters and an extra line shift at the end of the cc-file):

NDUMP 1

TDUMP 40

NDUMP 2

TDUMP 55

This gives 2 dumps at 40 and 55 seconds that can be used to restart the calculations.

3 RunManager - FLACS-CFD 222


File Tools Options Help Language



I B


Directory


Job number


Status


Disk Space


Add directory


▼ C:\Fl_ACS\Ex amp les\ex 04_d i spersi on\ Q


0 200001


C:\FI_ACS\Examples\ex03_explosion\

110101


533.04 KiB (Estimated)


Actions on checked jobs


Parameters


7.59 MiB (Estimated)


Calculate porosity

1.30 MiB (Estimated)

Simulate

X Abort simulation

/、Suspend/Stop simulation

Enter FLAGS Parameters

Resume simulation

C:\Fl_ACS\Examples\ex01_explosion\

100001

BLOCKED: |    0|

ABORTED: |    0|

Connect to FLACS C oud...

□ Setup file

Figure 7.10: Defining the cc file for dispersion simulation


NDUMP 1

TDUMP40

NDUMP 2

TDUMP 55


Start the simulation by clicking on the job and clicking simulate in the FLACS-CFD RunManager.

The most important result from this simulation is the gas cloud distribution. It can be studied in Flowvis. Cut plane plots of the gas cloud at times 40 s and 55 s are shown below. The concentrations are plotted in the flammable range for natural gas (i.e. between 5 % and 15 % natural gas).

Figure 7.11: Gas cloud distribution in the flammable range at time 40 seconds.

Figure 7.12: Gas cloud distribution in the flammable range at time 55 seconds.

In explosion simulations, one can compute the effect of igniting the realistic gas cloud that was calculated in a dispersion simulation as described above. To this end, copy the FLACS-CFD input files to a new job number (or use CASD to save the job with a new number). Dump the dispersion results at two discrete times: 40 s and 55 s. The gas cloud at 40 s is used to start an explosion simulation.

Use Flowvis to find a suitable ignition position e.g., make a contour plot (2D cut plane) of FMOLE or ER in the leak plane (Z = 2.4 m) to find regions where the concentration is close to stoichiometric (this is expected to lead to the worst-case explosion pressure). In this case, the figure above suggests an ignition position of (23, 4.5, 2.4) m. Certain changes need to be made to the scenario and the grid to make them appropriate for an explosion simulation. The following steps should be followed:

on the flammable gas cloud volume that is output from the dispersion simulation. Cells between the core domain boundary and the edge of the total simulation domain should be stretched by a factor of 1.2. Note that the total simulation domain may have to be extended to meet the grid recommendations. If the scenario is opened in CASD, then these grid changes can be made using Quick grid from the Grid menu.

After following the steps above, click on the job in the RunManager (if it is not visible, click on rescan directory). Click Parameters and define a cc-file. The cc-file should contain only one line (remember to include an extra line at the end):

NLOAD 1

The last step before running the explosion scenario is to generate a new rd-file for starting the calculation based on the dispersion job. This transfers the required information from the dispersion grid (job number XXXXXX) to the explosion grid (job number ZZZZZZ).

Linux: In a terminal window, type:

> run rdfile rdXXXXXX.n001 rdZZZZZZ.n001

(make sure that you are in the correct directory).

Windows: In a command window, type:

> rdfile rdXXXXXX.n001 rdZZZZZZ.n001

Start the simulation by clicking on the job and clicking simulate in the RunManager.

Use Flowvis to analyse the results and generate plots. A scalar time plot of pressure at all monitor points is shown below. The maximum pressure of 1.3 barg occurs at t = 40.34 s at monitor point 1.

Figure 7.13: Overpressures at monitor points as a result of the explosion of the dispersed gas cloud at t=40 seconds

Figure 7.14: Geometry for pool spread simulation

It is recommended to start out with an empty directory for storing the files.

Linux:

Make a distinct directory (DIRECTORY NAME) in which you perform the exercise:

Move into this directory: > cd DIRECTORY_NAME

Copy the geometry files (notice the space before the ”.”).

Start up the FLACS-CFD RunManager: > run runmanager

Windows:

In the RunManager, use Add Directory to find the directory that contains the geometry files. Use RunManager Tools CASD (or click the FLACS-CFD pre-processor icon). Open the file 600000.caj (and ignore any error messages that appear). The geometry is a simple model of an LNG terminal. Consider the following case:

Remarks:

600000.caj is the case that should be used for learning purposes. Case 600001 contains the same geometry, but it is made ready for simulation.

First, a Simulation Volume must be defined. The wind comes from the south, aligned with the Y axis, and the undisturbed wind field must be set at a certain distance upstream of the LNG terminal. One is most interested in the gas cloud on the terminal, but also in high concentrations further downstream should be captured. In the X direction, the domain should cover the area the pool can spread and the volume the cloud may fill in the cross-wind direction. In the Z-direction, the simulation volume should include the surface, the LNG terminal and some space above. Note that LNG vapour is heavier than air.

In the current example, a manual grid setup is demonstrated (i.e. without the Quick Grid tool). The following Simulation Volume is used: xmin= -50 , xmax= 90, ymin=-60, ymax=120, zmin=-1, zmax=40. In the X-direction, initialise a 1 meter grid: choose Grid Region 140. Fine grids give more accurate results and it is recommended to use a grid spacing of about 1 meter or less in the X- and Y-direction for pool simulations in the areas where the pool will spread. It may not be easy to forecast where the pool will spread, but some reasoning may be possible when the leak position and obstacles are known. A 0.5 meter grid is recommended in the near-field of the leakage location (X=28). Use CTRL + arrow keys to define the region 22 m – 32 m and set the number of control volumes of the selected region to 20. Smooth the grid, see Smooth. Stretch the grid for X 70 m and X -30 m.

Change to Y-direction (Grid Direction Y direction) and generate a 1 m grid (Grid Region 180). To get a 0.5 m grid around the leak location, use CTRL + arrow keys to define the region -5 m – 5 m and set the number of control volumes to 20. Stretch the grid towards the boundaries for Y 30 m and Y -30 m. Change to Z-direction (Grid Direction Z direction) and generate a 1 m grid (Grid Region 41) Just above the pool, a 0.25 m grid is desirable. Select the region Z = 10 – 13 m and increase the number of control volumes from 3 to 12 in this region. Then smooth the grid. Stretch the grid above the geometry (Z=17 m) towards the top boundary.

The grid now has about 460000 control volumes and the porosities should be calculated. Remember to save the scenario.

To create a pool scenario select 'Simulation type' Pool in CASD.

Use MOUSE+LEFT to select POOL D, FUEL, FMOLE, T, and VVEC. This will give 3D field outputs for the pool depth, that can be used to visualise the pool, FUEL and FMOLE which give the mass fraction and volume fraction (concentration) of the vapour, T, which is the gas temperature, and VVEC, which is the velocity vector.

Set

This is a dispersion scenario with wind at 3 m/s from south and neutral atmospheric conditions. Therefore YLO is the inflow boundary and YHI is the outflow boundary. The flow is parallel to the X boundaries and the ZHI boundary and WIND can be used for these boundaries, too.

WIND DIRECTION=(0,1,0).

The settings for the boundary and initial conditions for the wind field can alternatively be produced with the wind wizard: in the Scenario Settings click on Run Wizard and choose Wind Wizard. The setup for the current case is as shown in the figure below.

Figure 7.15: Wind wizard settings for the pool spread case.

To get a wind field of 3 m/s at 10 meter height and neutral atmospheric boundary conditions, set:

No ignition is wanted. Set TIME OF _ IGNITION larger than TMAX, for example

TIME OF IGNITION=9999.

Define the gas monitor region to cover the volume above the deck (i.e. X in (-35,35) m, Y in (-25,25) m, and Z in (11,17) m).

If you are a relatively new FLACS-CFD user then it is recommended to use the Pool section of the scenario menu in CASD (set the ”Simulation type” under ”Scenario Settings” to ”Pool”, or right-click in the scenario menu to enable the Pool section). The menu, and the settings and keywords used to configure a pool simulation, are described here.

The following setup is used in the example:

Figure 7.16: Pool setup in the scenario menu (left), pool leak data (right).

The above settings correspond to the following setup of a spreading pool with non-uniform pool temperature in the POOL section in the cs-file. (The POOL section in the cs-file contains more parameters but the scenario menu in CASD only shows a subset of these unless Show advanced is enabled by right-clicking in the view.)

Property name

Property ID

Value

Description

Non spreading

STATIC POOL

0

This scenario models a spreading pool, and not a non spreading pool

Uncoupled pool fire model

POOL FIRE UNCOUPL

D0

Enable to use the uncoupled pool fire model instead of the coupled one

Start time

START POOL

5

Pool begins 5 seconds after the simulation starts in order to establish the wind field

Initial mass

MASS POOL 0

0

No initial pool mass

Mass rate

DMDT

300

Pool leakage rate [kg/s].This value is overridden by the pool leakage file

Property name

Property ID

Value

Description

Position

POSITION

28 0 20

(X, Y and Z position of the centre of the leakage area. Z position is used to search downwards until solid ground with space above is found, that is PORZ(K) >= 0.5 and PORZ(K+1) 0.5. In this case, Z should be located above the geometry. If a spill on the sea is considered, Z should be located just above the sea surface, see Setting the pool position.

Inner radius

RAD I

0

Outer radius

RAD O

2

Radius of the leakage area [m]; to get a circular shape for the spill, it is recommended to set RAD-0 3Ax. In this case is RAD_0 = 4Ax.

Ground temperature

T SOIL

293

Ground temperature [K]

Heat sun

HEAT SUN

400

Heat from the sun [W/m2]

Surface roughness

ROUGH L

0.005

Ground type

POOL GROUND

”CONCRETE,WATER[:: 1 0.5]”

- Concrete everywhere except for the Z-region (-1 m – 0.5 m), where there is water

The pool leakage file cl000000.POOL overrides DMDT from the cs000000.dat3 file, see pool leakage file. The time in cl000000.POOL is relative to START POOL in cs000000.dat3. A constant release rate (300 kg/s) for 10 seconds and then a linear decrease in the release rate during the next 10 seconds is defined by:

’POOL LEAK FILE’

2

’TIME [s]’ ’DMDT [kg/s]’ 0.0300.0

10.0300.0

20.00.0

200.00.0

The data for the pool leak file can also be entered in CASD: right click in the scenario menu and enable the Pool leak menu, which allows to enter the rates (right-click in the menu to enter new lines), see the screenshot above.

The most important result is the gas cloud distribution. It is also important to plot the pool shape, pool mass and evaporation rate in order to verify the source term and to ensure that the pool spreads as expected. In the figures below, volume plots are used to visualise the pool and the gas cloud. In addition to the case described above, a release on the sea at the same X and Y position has been considered. Pools are plotted for depths in the range 1 - 20 mm and gas concentrations above LFL/2 are shown. It is recommended to turn off trilinear interpolation (Plot Specification Trilinear) when plotting POOL D.

X(m)

Job=000000. Var=POOL_D (m). Time= 74.996 (s). X=-48 : 73, Y=-48 : 48, Z=2 : 19 m

Job=000000. Var=FMOLE (m3/m3). Time= 74.996 (s).

X=-48 : 73, Y=-48 : 48, Z=-0.5 : 19m

Figure 7.17: Pool spread on deck. Pool (left) and LFL/2 gas cloud (right).

Z(m)


Z(m)

A

20-

Job=100001. Var=POOL_D (m). Time= 29.999 (s).

X=-48 : 73, Y=-48 : 48, Z=0.3 : 31 m

Figure 7.18: Pool spread on the sea. Pool (left) and LFL/2 gas cloud (right).


20-

Job=100001. Var=FMOLE (m3/m3). Time= 29.999 (s).

X=-48 : 73, Y=-48 : 48, Z=-0.8 : 31 m


In the figures below, pool mass, pool area, and evaporation rate per square meter are shown for pool spreading on concrete (deck) and pool spreading on water (sea).

Figure 7.19: Pool evaporation on concrete.


Figure 7.20: Pool evaporation on the sea.


The pool model is two-dimensional in space and a crucial point is the detection of the underlying solid surface seen by the pool model. At present, the surface on which the pool can spread is detected by searching downwards from a vertical position, Z ,for all X and Y positions. A solid surface is detected if:

This means that if Z is located in the open, then the first cell with PORZ < 0.5 below Z determines the surface elevation.

It follows from the inequalities above that walls and bunds must be at least 0.5AX wide in order to be found by the underlying-solid-surface detection algorithm. An example where bunds not are detected is shown in Figure Bunds not detected. Possible solutions are to increase the bund thickness and to refine the grid.

Figure 7.21: Bunds not detected because PORZ>0.5.

If Z is given a high value, the pool sees equipment etc. as solid obstacles even though there is a gap underneath the equipment where the pool can spread, see Gap under tanks. The solution is to set a lower value for Z, for instance just above the green surface.

Figure 7.22: Gap under tanks not detected.

It should be mentioned that if no underlying solid surface is detected by searching downwards, then an upwards search is carried out from Z. The top of tank 1 in Figure Gap under tanks will be detected for a low Z value.

Difficulties may be encountered when there are several gaps, for instance if there are several decks. In the example in Figure Unwanted depression and Figure No gap, there is no obvious value for Z. If Z is located above the tanks, the pool will not flow under tank 1. If Z is just above the surface, an unwanted depression is generated instead of an obstacle at tank

Warning:

The pool model does not detect pool depth correctly when there are no grid planes beneath the lowest surface in the geometry. The solution to this problem is to extend the grid below the lowest surface on which the pool can occur.

FLACS-CFD automatically calculates properties for mixtures of species known to it, and mixtures including hydrocarbons from methane up to dodecane can be defined as fuel in FLACS-CFD (see the section on Gas composition and volume).

Attention:

C5 to C10 alkanes have the same laminar burning velocity as butane; C11 and C12 should not be included in a combustible mixture. Cf. the section on potential problems with heavy hydrocarbons.

A simplification of the definition of the combustible mixture can be obtained by replacing C5+ by C4 (butane) in the way it was suggested before C5+ were available in FLACS-CFD, namely by conserving the number of C's, e.g., 1 mole of C8 becomes 2 moles of butane, since the oxygen consumption (and FLACS-CFD interpolation rules) depends on the number of Cs. This approach underlies the same limitations mentioned above. In any case, one has to assess how much of the heavy hydrocarbons one wants to include, since at some stage they will remain liquid and rain out if the pressure is low (and/or the fraction of lighter components is low).

As far as inerts are concerned, water vapour should have an effect in between what is seen for CO2 and N2 as an inert. For CO2 typically 4 % in the final explosive mixture (including air) would reduce pressures by a factor of 2, whereas roughly 8-9 % added nitrogen will be required. One could therefore assume that approx. 6 % added water vapour in the final gas-air mixture would have a similar effect, reducing explosion pressures by a factor two. The background humidity in air, which can of course vary with temperature and climate, is not considered when doing explosion modelling, i.e. FLACS-CFD is calibrated for a typical relative humidity level (and variations from this may be part of uncertainty in predictions).

Note that nitrogen cannot be chosen as a gas. If one wants to specify N2 in a fuel mixture, the easiest way will be to redefine the AIR so that your final composition has the correct amount of nitrogen.

For dispersion simulations, nitrogen can be replaced with a mixture of other gases (CO or ETHYLENE has the same molecular weight) or a user-defined gas can be defined.

It is recommended to start with an empty directory for storing the files.

Linux:

Make a distinct directory (DIRECTORY NAME) in which you perform the simulation:

Move into this directory:

Copy the geometry files (notice the space before the ”.”).

Edit/verify the cs-file with your favourite editor.

Start up the FLACS-CFD RunManager (assuming that you have set up an alias for the run script):

Windows:

C:\Program Files\Gexcon\FLACS-CFD_22.2\doc\examples\ex05_fire\*00 0 01* (00001 means all files containing the text ”00001”).

To create a fire scenario select the corresponding simulation type (fire) in the CASD Scenario menu. Enable the write all variables check-box to get all fire related single field variables.

Define the monitor point direction (required to calculate incident radiative flux) along with the position and output variables. The monitor point direction is specified as a vector and determines the heat flux radiometer direction.

Choose the fire-related variables (SOOT, H2O, CO2, CO, VFSOOT, VFH2O, VFCO2, ABSCOF, RADSRC, QRAD, QCONV, Q, QDOSE) required for the analysis to view the results for the relevant monitor points.

Left-click to choose TWALL, SOOT, H2O, CO2, CO, VFSOOT, VFH2O, VFCO2, ABSCOF, RADSRC, QRAD, QCONV, Q, QWALL, QDOSE. This will give 3D field output of the variables required for fire simulations.

Right-click into this scenario menu and enable show advanced. Then apply the following settings:

The default boundary condition for FLACS-Fire simulations is NOZZLE. The boundary condition WIND can be used to model a specified wind field at selected boundaries.

To obtain better stability, set the initial turbulence to be low:

Leave the other parameters unchanged.

Always use the leak wizard to specify leaks. There are two ways to represent leaks: point leaks and area leaks.

According to the grid recommendations, the grid should be refined around the leak. Keep in mind that only the grid cell containing the leak and one neighbouring cell on each side needs to be refined and that the grid spacing should be smoothly increased to the prevailing grid spacing. For coupled pool fires, a fine grid is required in the vicinity of the pool surface to anchor the flame, cf. the sections on LNG Pool Fire, Pool spread simulation and Coupled pool fires.

Typical evaporation rates for some of the species in the FLACS-CFD database can be found in the section on Source term modelling for pool fires. For uncoupled pool fires these values may be used to mimic an evaporation pool, by using them as leak rates of an area leak. Another choice is to employ the coupled pool fire model. Here the evaporation rate is calculated by the pool model using a coupling with the radiative heat transfer from the flame to the pool.

For a fire simulation, you must specify the location and size of the ignition source and also the time and duration for the ignition.

This sub-menu allows you to select from the available radiation models and specify their parameters (see radiation scenario).

In this menu the use of radiative heat transfer to the pool can be chosen and the threshold for the radiative heat transfer can be set. For pool fires in general the FIRESWITCH should be set to 2 under Combustion settings.

FLACS-CFD can model uncoupled and coupled pool fires:

Whether a pool is modelled as coupled or uncoupled, it is recommended to use FIRESWITCH=2.

This sub-menu allows you to select one of the available combustion models. The default and recommended choice is the Eddy Dissipation Concept (EDC). As the EXTINCTION option is still under development it should be deactivated. Set the FIRESWITCH to 2 for both jet and pool fires.

This setting allows to select an appropriate soot model. The default and recommended choice is the Formation-Oxidation model.

The conduction model in FLACS-Fire is under validation. It is recommended not to use the conduction model in this version.

To start the FLACS-Fire simulation use the following commands:

Windows:

Start the simulation in the RunManager by marking the job and clicking simulate.

Linux:

Start up the FLACS-Fire simulation (on your local computer):

> /usr/local/Gexcon/FLACS_v22.2/bin/run flacs version fire 000004

If a stack overflow problem occurs see how to Increase the stack size on Linux.

This section presents various test cases for FLACS-Fire.

The SINTEF Impinging jet fire (Wighus & Drangsholt, 1993) from high pressure leakages is representative of a severe hazard on offshore platforms and in onshore process plants. The experiments were undertaken to get better knowledge of the effects of an impinging jet fire regarding heat load and the erosive effect from high temperature and a velocity jet.

The propane jet enters horizontally into a box-like target, standing at an angle of 60 or 90 degrees to the jet axis. The dimensions of the box are: width W = 1.5m, height H = 1.5m, and depth D = 0.45m. The jet axis is positioned centrally at 1/2 or 1/4 H, and at distances of L=1.0m, 1.5m, or 2.5m from the wall of the box. A pipe with a diameter of 278.0mm was mounted across the front of the box in three of the tests, at 1/2 or 3/4 of the box height.

Table 7.2: Summary of SINTEF Impinging jet

Configurations

SINTEF impinging jet

Dimensions of the box

W=1.5 m, H=1.5 m, D=0.45 m

Fuel

Propane

Jet velocity

260 m/s

Jet distance

2.5 m

Jet Height

0.75 m

Jet angle

90 degree

Computational details:

In the Figure below the geometry configuration, for the SINTEF impinging jet fire case is shown, including the grid. The number of grid cells used is 57,330. The total number of rays fired is 108.

Figure 7.25: Calculation domain and grid distribution


Grid:

• Dimensions of the computational domain (m): Xmin


=-5.0,


Xmax


= 5,


Ymin


= -5.0,


Ymax


= 5.0,


Zmin = -0.5,


Zmax


= 10.0


• Total number of cells: 57,330

• Size of grid cells (at the leak location): 200 x 41 x 41 mm

Monitor points:

MONITOR_POINTS

INSERT 1

0.02

0

0.375

DIRECTION

0

0

0

INSERT 2

0.1

0

0.75

DIRECTION

0

0

0

INSERT 3

0.02

0

1.125

DIRECTION

0

0

0

INSERT 4

0.02

0

1.47

DIRECTION

0

0

0

INSERT 5

0.415

0

1.47

DIRECTION

0

0

0

INSERT 6

0.01

-0.1

1.125

DIRECTION

0

0

0

INSERT 7

0.415

-0.1

1.52

DIRECTION

0

0

0

INSERT 8

0.01

0

1.125

DIRECTION

0

0

0

INSERT 9

0.01

0.1

1.125

DIRECTION

0

0

0

INSERT 10

0.9

0

0

DIRECTION

0

0

0

INSERT 11

0.9

0

0.15

DIRECTION

0

0

0

INSERT 12

0.9

0

0.3

DIRECTION

0

0

0

INSERT 13

0.9

0

0.45

DIRECTION

0

0

0

INSERT 14

0.9

0

0.6

DIRECTION

0

0

0

INSERT 15

0.9

0

0.75

DIRECTION

0

0

0

INSERT 16

0.9

0

0.9

DIRECTION

0

0

0

INSERT 17

0.9

0

1.05

DIRECTION

0

0

0

INSERT 18

0.9

0

1.2

DIRECTION

0

0

0

INSERT 19

0.9

0

1.35

DIRECTION

0

0

0

INSERT 20

0.9

0

1.5

DIRECTION

0

0

0

EXIT MONITOR_POINTS

SINGLE_FIELD_SCALAR_TIME_OUTPUT

NT 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20

NQRAD 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20

EXIT SINGLE_FIELD_SCALAR_TIME_OUTPUT

Numerical parameters:

Boundary conditions:

Initial conditions:

Leaks:

Radiation:

Regarding radiation modelling with the Discrete Transfer Method (DTM)

Combustion:

Soot:

Leaks:

Results:

The figures below shows flame temperature and heat flux at box like target for the SINTEF impinging jet fire case. .


Figure 7.26: 3D plots of temperature in SINTEF impinging jet fire case with default settings


Figure 7.27: 3D plots of total heat flux


Figure 7.28: 3D plots of radiative heat flux


Figure 7.29: 3D plots of convective heat flux

Discussion:

Problem description:

This large-scale experiment consists of an LNG pool on the sea surface (Raj, 1979; Schneider, 1979; Schneider, 1980). Measurements and observations were done for radiative heat flux, burn rate, flame geometry, and flame speed. Other large-scale experiments have also been performed, both on water and land (Luketa-Hanlin, 2006). A principal difference between LNG pool fires on land and water is the height of the flame, which is about a factor of two greater on water than on land. The reported flame length in the experiment was between 25-55 meters.

Grid:

First a simulation volume must be defined. There is no wind field in this simulation, hence the domain in the XY-plane should be equally spaced around the leak. In the X- and Y-direction, the domain should cover the area of the pool surface plus twice the pool diameter to each side of the area covering the pool. In the Z-direction, the simulation volume should include 6-7 times the diameter of the pool. The following simulation volume is used in this example: xmin= -45 , xmax= 45, ymin=-45, ymax=45, zmin=0, zmax=100. Finer grids give more accurate results (cf. Coupled pool fires for grid guidelines) and it is recommended to use a grid spacing smaller than 1 meter in the X- and Y-direction in the area of the leak. Use square cells. It is not easy to know in advance how high and wide the flame will develop, so in order to avoid problems on the boundaries, the simulation volume should be made sufficiently big (see above for guidance). A pool fire will have so-called puffing. To resolve this, the numerical grid needs to be sufficiently fine (with a too coarse mesh the flame will have a more cylindrical shape).

In this example, a grid can be chosen as follows: In the X- and Y-direction, initialise a 0.5 meter grid. From the boundary of the leak area surface (Z=0), stretch the grid to the boundaries. For the Z-direction, start with a grid spacing of 0.5 meters and stretch the grid from Z=50 meters. Keep a maximum grid spacing of 2 meters to the upper boundary. The grid has now about 590000 control volumes and the porosities must be calculated. Remember to save the scenario.

Simulation and output control

Boundary conditions:

Initial conditions:

Gas composition and volume

Ignition

Set an ignition volume with dimension 101020 meters in X-Y-Z direction at the centre of the XY-plane and from Z=0.

Leaks and leak file

Set up an area leak with a diameter of 15 meters, with the leak pointing upwards. Gaussian profile and elliptical shape, 0.2kg/(m2 s).

Radiation:

Regarding radiation modelling with the Discrete Transfer Method (DTM)

Combustion:

Soot:

Conduction:

Results:

The figure below shows a temperature plot from the simulation of the U. S. CG China Lake tests. The results shown here account for radiative heat loss. The published flame height is between 25 and 55 meters, and the model results are in the same range.

Run:000002

Ivar: T |Time 61995.65 ms (62)|

Figure 7.30: Temperature plot of the U.S. CG China Lake tests LNG pool fire.



Discussion:

The default model in FLACS-CFD for pool fires is the “uncoupled pool fire model”. In the uncoupled pool fire model it is assumed that there is no feedback from the pool fire on the burning rate. A uniform burning rate is instead prescribed based on empirical correlations. The uncoupled pool fire model is most suitable for pool fires where the assumption of a uniform fixed evaporation rate holds, i.e. in relatively open areas, and for pools that remain approximately circular. For other cases and especially for under-ventilated scenarios, it is recommended to use the coupled pool fire model.

For this model, FLACS-CFD prescribes the burning rate based on the mixture, the effective pool diameter, and wind conditions. The table below lists the burning rates used based on (Rew, P.J., Hulbert, W.G. (1996)). If the burning rate is not tabulated, FLACS-CFD employs the Burgess correlation from the Yellow Book for predicting the mass burning rates of uid flammable materials under ambient conditions (see EFFECTS user and reference manual) The ultimate values are then corrected for both the pool size and wind speed (Bubbico et al. (2016)).

The table below lists typical evaporation/burning rates for a selection of flamable liquids for large pool fires, based on (Rew, P.J., Hulbert, W.G. (1996)).

Table 7.3: Summary of typical evaporation/burning rates for selected liquids (Rew,1996)

Material

Mass burning rate [kg/(m2 s)]

Acetone

0.038

Benzene

0.085

Butane

0.11

Crude oil

0.051

Diesel

0.054

Ethane

0.141

Ethanol

0.02

Material

Mass burning rate [kg/(m2 s)]

Fuel oil

0.034

Gasoline

0.067

Heptane

0.081

Hexane

0.075

Hydrogen (liquefied)

0.161

JP4

0.056

JP5/kerosine

0.063

LEG

0.14

LNG/Methane

0.141

LNG/Methane (water)

0.282

LPG/Propane

0.118

LPG/Propane (water)

0.256

Methanol

0.02

Naptha/Pentane

0.095

Octane

0.081

Toluen

0.066

Xylene

0.09

The main difference when running the coupled pool fire model in FLACS-Fire is the way evaporation is modelled. In the uncoupled pool fire model the evaporation rate is either read off from a table or approximated via an empirical correlations. For the coupled pool fire model the pool model calculates the evaporation from the pool by a heat transfer balance including heat from the flame. The pool setup parameters must be specified correctly. Ignition must be set later than the startup time for the pool if persistent ignition is not active, that is DURATION OF IGNITION=0.

The results are grid sensitive. A fine grid in the vicinity of the pool surface is required to anchor the flame properly. It is recommended to do some grid sensitivity studies for the area close to the pool surface to check that the physics of the fire is captured. In the example pool spread simulation a sensible grid is described. When running with the coupled pool fire model it is recommended to use cubical cells close to the pool surface. The mixing region above the pool, in the z-direction, is sensitive to the grid resolution. About 1 m above the surface the grid may be stretched to bigger cells, but keep cell sizes within 1 m. Above the assumed flame height the grid may be stretched further.

The computational domain should be at least two pool diameters to each side of the leak in the XY-plane. If a wind field is applied, then the domain should be at least 4 pool diameters in the downwind direction. In the vertical direction, the domain should be at least 6 pool diameters. Since pool fires result in puffing (oscillatory behaviour of the flame), a fine grid is needed to capture this effect. It is not easy to predict what the grid spacing should be. It depends on what one is trying to accomplish. A mesh sensitivity study should always be performed; start with a relatively coarse mesh, and then gradually refine the mesh until the results show small differences. A general recommendation is to use equal-sized grid cells in the horizontal plane covering the pool area and at least 10-15 cells across the characteristic diameter of the flame D (Lin, 2010):


Q

Pg cpTg "g


(2/5)

D


(7.1)

Here, Q [kJ/s] = pool fire heat release, p^ [kg/mA3] = ambient air density, c[kJ/kg*K] = constant pressure heat capacity of the fuel, T[K] = ambient air temperature, and g [m/s2] = gravitational acceleration.

The spreading pool model allows the spill to move in the XY-plane. The non-spreading and spreading pool models may be used for the same study given that the spreading pool is restricted from moving by including extra obstructions in the geometry (bund).

The coupled pool-fire model has been validated for fixed size pool fires. Moving combusting spills is possible to model through pool model 3, but this is still under validation, hence no recommendations for the grid are given here.

As most of the (jet) dispersion guidelines for the time step and grid also apply for jet fire scenarios, it is straightforward and quick to convert an existing FLACS-CFD dispersion scenario to a FLACS-Fire scenario by the following steps:

•Q

•T

•Q

•T

to force DTM-recalculation and result data export once per simulated second. Setting the DTM MOD TIME and DTPLOT to the same value will synchronise the DTM calculations with the 3D output in the video and look best when visualising 3D radiation values in a video

The visualisation of flames and smoke has been greatly simplified in FLACS-CFD 21.3. with automatic defaults for both and it is recommended to use those settings.

For FLACS-CFD ventilation, dispersion and explosion simulations calculating times are a function of, among others, the number of grid cells, the time step length and the simulated duration. Fire simulations are very similar to dispersion simulations, however they take longer for the following reasons:

For identical simulation durations; fire simulations will take longer to run than comparable dispersion simulations; typically about 1.2x to 10x longer. However, often the time of interest for fire simualation can be much shorter than for dispersion simulation (e.g. when only flame positio or quasi-steady state heat radiation results are needed), in which case the time to run simulations may still be less than for similiar dispersion simulations.

This section aims at giving a better understanding of the factors that influence calculation times and how changing various DTM settings will impact the calculation times and to lesser extent memory footprint. In most cases it should be possible to obtain accurate results with FLACS-Fire within a few hours, up to a few days for very large simulations.

Note:

The RADI DTMHy Total line in the FLACS CALL PROFILE section in the simulation log file shows total time and relative time used by the DTM routines. In cases where the DTM part of the calculation in the simulation takes a signigicant amount of time (e.g. more than 25%-50%, see note below) the following steps can be taken to reduce calculation time:

The time needed for the DTM part of the calculations, scales linarily with the number of rays defined in DTM _ RAYS setting in the cs-file. Fewer rays will result in coarser heat radiation results within the DTM domain (e.g. more flower pattern effect), but shorter calculation times. In most cases the default number of rays will be optimal.

The time needed for the DTM part of the calculations, scales linarily with the frequency of DTM calls in the DTM ITER or DTM TIME setting in the cs-file. Less frequent DTM iterstion rays will result in capcturing less of the dynamic behaviour of the flames, but shorter calculation times. In most cases the default number of DTM iterations will be optimal.

The size of the DTM domain influences the calculatoin time signficiantly. With the default settings, the DTM domain size is automatically adjusted around the flame, this means that when the flame gets larger the time needed for the DTM calculations will also increase. When the DTM domain size has been set manually, reducing the DTM domain when possible will help reduce caluclation time.

For most FLACS-Fire simulations there currently is very little benefit of using the incompressible solver. In addition, most of the validation has only been done for the compressible solver. It is therefore recommended to only use the compressible solver for fire simulations.

FLACS-Fire can limit the calculation of the DTM radiation model to only a part of the total simulation domain. This allows simulations to run much more quickly, and in combination with the optional far-field model generates smoother contours in the far field. For most scenarios, the default settings should give an optimal balance between calculation time and accuracy and validity of the results. However, in some cases you might wish to deviate from the default settings. Below is a summary of the relevant options and information for which situations they are most suitable. Note that these settings are only available when enabling the Advanced options in the radiation tab (right-click to enable).

Possible settings of DTM DOMAIN CONSTRAINTS:

For both automatic settings, the DTM domain will be limited and the DTM ray effect reduced; typically 100 DTM rays will be sufficient.

FAR _ FIELD MODEL

For a dispersion study following a leak in a process area, the main parameter is the size of the flammable gas cloud. To evaluate the hazard of a given gas cloud, Gexcon has developed methods for natural gas that aim at estimating an equivalent stoichiometric gas cloud with comparable explosion consequences; these methods have been developed in order to reduce the number of simulations that need to be carried out to do a risk study, and the principles should be applicable to other gasses as well. For uncongested explosions, the initial turbulence characteristics of the gas cloud are also important. Gexcon has therefore carefully determined the most appropriate values to use when describing the initial turbulence characteristics for an equivalent stoichiometric gas cloud, see Initial turbulence for the equivalent gas cloud.

The size of the equivalent stoichiometric gas cloud at the time of ignition is calculated as the amount of gas in the flammable range, weighted by the concentration dependency of the flame speed and expansion. For a scenario of high confinement, or a scenario where very high flame speeds (faster than the speed of sound in cold air) are expected (either large clouds or very congested situations), only expansion-based weighting is used (denoted as Q8). For most situations lower flame speeds are expected and the conservatism can be reduced. Here a weighting of reactivity and expansion is used (denoted as Q9). The definitions of the Q8 and Q9 equivalent volumes are given in Section Q8 and Q9 output.

The Q9 cloud is a scaling of the non-homogeneous gas cloud to a smaller stoichiometric gas cloud that is expected to give similar explosion loads as the original cloud (provided the shape and position of the cloud are chosen conservatively, as is the ignition point). This concept is useful for QRA studies with many simulations, and has been found to work reasonably well for safety studies involving natural gas releases (NORSOK, 2001).

The Q9 concept has also been applied to hydrogen systems for the FZK workshop experiments and has been found to give reasonably good predictions. Details can be found in (Middha et al., 2006; Middha et al., 2008).

As a practical guideline, it is recommended to choose the shape of the cloud such that it will give the maximum travel distance from the ignition location to the end of the cloud for smaller clouds. For larger clouds, end ignition scenarios with longer flame travel should also be investigated. The cloud should be made as a hexahedral box with assumed “planes of symmetry” towards confinement. The aspect ratio for a free cloud should be 1:1:1, for a cloud towards the ceiling 2:2:1, towards the ceiling and one sidewall 2:1:1, etc. For a free jet in a less confined situation, the jet momentum will usually dominate the mixing of the jet until the fuel concentration has become lean, unless the wind is very strong. The cloud should be assumed to be located a small distance downwind of the jet, if possible conservatively towards obstructions/walls. For highly buoyant gases such as hydrogen, it can always be assumed that a confined or semi-confined cloud is located near the ceiling or below any other horizontal confinement (a possible deviation from this may be large liquid hydrogen releases in hot and dry surroundings).

The initial turbulence conditions are likely to have a very small effect for strongly congested simulations since turbulence will be generated quickly by the geometery in the explosion region. However, for explosion scenarios with little congestion near the ignition location, it is important to describe the initial turbulence conditions appropriately. The settings in the table below are recommended if the turbulence characteristics of the gas cloud are not known (these are the default values for gas explosion simulations). The turbulence length scale is proportional to the diffusion of the cloud, so if it is set too high in the initial conditions then it is possible that parts of the cloud that are distant from the ignition will have dissipated before the combustion reaches them. It is therefore recommended that the initial turbulent length scale is not set to be higher than the default value, even in cases for which it is known to be higher in reality. The turbulence in a cloud that has some initial turbulence but has a characteristic velocity of 0 will reduce very quickly. It is therefore important that ignition happens immediately if it is intended that the cloud has turbulence when it is ignited (see Ignition of the equivalent gas cloud for details about setting the ignition appropriately).

Note that while 200 m/s is a reasonable estimate for the velocity of a jet release, FLACS-CFD is sensitive to the product of the characteristic velocty and the relative turbulence intensity, rather than to the characteristic velocity itself.

Table 7.4: Recommended intial turbulence settings for gas explosions.

Setting

Value

Characteristic velocity

200 m/s

Relative turbulence intensity

0.3

Turbulence length scale

0.05

These recommended settings were calibrated using data from three experiment campaigns, including 20 explosion experiments. The figure below compares the maximum pressure measured in the experiments with the maximum pressure that was simulated using a combined dispersion-explosion simulation, (this configuration is anticipated to achieve the most accurate simulation, see Combined dispersion and explosion simulations), and using two equivalent clouds: one using the previously recommended initial turbulence settings, and one using the new recommendations. The simulated pressures are co-located with the experiment measurement locations. The x-axis is the ratio of the maximum simulated pressure to the maximum measured pressure. Where FLACS-CFD underpredicts the maximum pressure, the ratio has a value less than one, and values greater than one represent overprediction. The y-axis shows the cumulative probability for the ratio. In previous releases of FLACS-CFD, it was recommended that the initial relative turbulence intensity and turbulence length scale be set to zero. This results in much higher probability of underprediction for the maximum pressure than when a combined dispersion-explosion simulation is run. When the new recommended values are used, the probability of underprediction is much lower and is similar to the probability for combined dispersion-explosion simulations.

When the results of a dispersion simulation are available, but a combined explosion-dispersion simulation is not (for example, if a dispersion simulation was used to calculate a cloud, which was then repositioned to simulate multiple explosion scenarios in different locations), then the initial turbulence conditions for the gas cloud can be read from the dispersion simulation output. The turbulence values will vary across the cloud, and gas explosion simulations in FLACS-CFD currently assume uniform initial turbulence conditions. In most cases, it is appropriate to set the initial turbulence for the explosion simulation to be equal to the maximum turbulence conditions from the dispersion simulation output, since this will result in the most conservative predictions.

A】qpqo」d ElBDlunu

Figure 7.31: A comparison of the maximum pressures measured in experiments with those from combined dispersion-explosion simulations ('Real cloud'), and from two equivalent cloud simulations, using the previously recommended settings, and the new recommendations. RTI and TL are the initial relative turbulence intensity and initial turbulence length scale, respectively.

For smaller clouds (the flame travels less than 1 m to the open boundary), ignition with maximum distance to the edges of the gas cloud is normally a conservative choice (for a cloud located in a corner, this means corner

ignition, not central ignition). This could be used to represent all scenarios. Alternatively, a distribution of several ignition points could be applied. For larger clouds, a homogenous distribution of ignition positions should be applied. It should be kept in mind that the gas clouds with the possibility of the longest flame travel are often the most dangerous ones.

For a quantitative explosion risk assessment the explosion simulations should be performed with various idealised clouds of variable size and typically using stoichiometric concentration. For the purpose of QRA, the distribution of ignition locations should be chosen to represent reality. If there are one or more highly likely ignition locations that dominate the ignition frequencies, these may be used. Otherwise, it should be assumed that a constant ignition source might lead to end ignition (where concentration reaches LFL), whereas intermittent ignition sources will be more arbitrarily distributed (with higher likelihood centrally in the cloud where concentrations are above LFL). For stratified clouds, end ignition will mean ignition in the lower end of the cloud.

Two ignition probabilities should generally be established (in case of hydrogen, the probability of spontaneous ignition should also be considered):

From the CFD calculations, the volume of the gas cloud with concentration between LFL and UFL will give the volume that may be ignited if exposed to an intermittent ignition source. This information should thus be related to the intermittent ignition frequencies defined. In the case of constant ignition source, the Q6 output from FLACS-CFD (or similar from another CFD tool) gives the cloud volume that was exposed to flammable gas concentrations for the first time last second. This information should be combined with the probabilities for ignition by constant ignition sources. Thus for each time step (or each 1 s) for every dispersion calculation, the probability of ignition from spontaneous, intermittent and constant ignition sources should be established, and this probability should be added to a gas cloud size class (based on corresponding Q8, Q9 or a combination).

If the gas cloud becomes rich (in a well-mixed state, but more gas available than needed to fill the volume with stoichiometric concentration) this may be represented either as a stoichiometric cloud or as a rich cloud with a slightly higher reactivity than observed. This can be done by using the flammable volume to establish the volume of the cloud and the flammable mass to establish its concentration.

As described above, for scenarios with high confinement or scenarios where very high flame speeds can be achieved, one should use the Q8 value instead of Q9. To evaluate this, several cloud sizes can be simulated to identify a critical cloud size, Qcrit, for which the flame speeds exceed e.g., 200 m/s. For clouds with Q8 < Qcrit, the weighting procedure above can be applied. For clouds with Q8 > Qcrit, one should apply the Q8 cloud as representative cloud size. For vented rooms and other situations with a significant confinement, a weighting between Q8 and Q9 volumes is suggested.

If the ventilation or a high-momentum leak (jet) creates significant turbulence in the region where ignition is expected, this turbulence should be defined as an initial condition for the CFD solver, see Initial turbulence for the equivalent gas cloud for a description of the initial turbulence settings.

Further details of the approach and a discussion of potential issues can be found in (Hansen, 2011).

Fire evolution and structural response are interconnected, and therefore the output from fire simulations can be useful as input to software that compute structural response. Such tools, which are often based on the finite elements method (FEM), usually support import from several file formats, and the FLACS-CFD Python API documentation includes an example script for exporting data to one of these format, i.e. the Abaqus ”.imp” format.

The geometry is set up as usual for FLACS-CFD, and the Grid guidelines should be followed to ensure that the grid and geometry meet the recommendations for a blast scenario.

Monitor points are set in the same manner as for other FLACS-CFD simulations, however FLACS-Blast treats all porosities as either one or zero, so monitor points should not be placed in cells where the porosity is 0.5, see the blast section in Modelling and application limitations.

FLACS-Blast does not include pressure panels; to measure the pressure at walls, place monitor points between the cell centre and the adjacent wall (but not on the wall itself). The pressure measured at the monitor point will be the same as the pressure at the wall. Be aware that if the grid is refined it may be necessary to relocate the monitor points. Therefore, it is recommended that monitor points are positioned sufficiently close to the wall that they are located between the grid-cell centre and the wall for the finest expected grid resolution.

The default settings are appropriate for most cases. If numerical instability occurs – a rare occurrence – CFLC and CFLV may be reduced by a factor of 2. However, other possible reasons should be ruled out first. The maximum time should be set to a physical value. Usually 0.2 seconds is enough time to capture the history of the blast across the computational domain. Longer times may be required for very large domains.

The PLANE WAVE boundary condition must be used with the blast simulator. See the boundary conditions section for more details. The computational domain should be such that the total volume is about 100 times larger than the volume of the initial explosive “balloon”. It is recommended to perform a sensitivity analysis to verify that the solution is independent of the domain size.

The explosive charge is defined using the following parameters:

Table 7.5: Variables that define the explosive charge for a blast simulation.

Variable

Description

POSITION

X, Y and Z locations of the explosive charge (centre of the “balloon”).

WEIGHT

Weight of the explosive charge in kg.

CONFINEMENT

Coordinate directions into which the blast will propagate from the initial high-pressure high-temperature region. Available options (= includes both + and - directions):

+X, -X, =X

+Y, -Y, =Y

+Z, -Z, =Z

For example, =X=Y=Z means the blast will propagate in the all directions. +X-Y means the blast will propagate in the +X and -Y directions only (i.e. the -X, +Y and Z directions are blocked).

TYPE

TNT or RDX.

Note:

The scenario files for this example can be found in the doc/examples/ex06 blast directory of your FLACS-CFD installation.

7.11.6.1 Problem description

The blast effects of an explosion of 0.8 kg of TNT on two adjacent structures and surrounding areas are simulated using FLACS-Blast. The structures are represented by blocks of the size 2.3 m x 2.3 m x 2.3 m. The minimum x, y and z coordinates of structure 1 are -3.45, 1.15 and 0 respectively, and for structure 2 are

1.15, 1.15 and 0. The gap between the structures is therefore 2.3 m. The TNT explosive charge is located

approximately 1.1 m from structure 1. The geometric setup is presented in the figure below.

Figure 7.32: Geometry for the blast simulation.

7.11.6.2 Computational grid

The computational grid contains 1,046,032 cells. Cubical cells of 0.1 m x 0.1 m x 0.1m are used in the region where accurate results are required, and are stretched towards the boundaries.

Monitor points are defined at the following locations:

INSERT

1

-2.

29

3.

46

1

.14

INSERT

2

-2.

29

3.

46

0

.19

INSERT

3

-1.

14

2.

29

0

.19

INSERT

4

-2.

29

1.

14

1

.14

INSERT

5

-2.

29

1.

14

0

.19

INSERT

6

-3.

46

2.

29

1

.14

INSERT

7

-3.

46

2.

29

0

.19

INSERT

8

-2.

29

2.

29

2

.31

INSERT

9

-3.

24

1.

14

0

.19

INSERT

10

-3.

46

1.

36

0

.19

INSERT

11

2.

29

3.

46

1

.14

INSERT

12

2.

29

3.

46

0

.19

INSERT

13

3.

46

2.

29

0

.19

INSERT

14

2.

29

1.

14

1

.14

INSERT

15

2.

29

1.

14

0

.19

INSERT

16

1.

14

2.

29

1

.14

INSERT

17

1.

14

2.

29

0

.19

INSERT

18

2.

29

2.

29

2

.31

INSERT

19

-0.

01

-4.

01

0

.01

INSERT

20

-5.

74

2.

29

0

.01

INSERT

21

-6.

89

2.

29

0

.01

INSERT 22  -8.19     2.290.01

INSERT 23 -11.49     2.290.01

INSERT 24  -0.01    -0.010.01

At all monitor points, the following variables are recorded: NPMAX, NPMIN, NPTIMP, NP, NPIMP.

The following variables are recorded for the 3D output: NPIMPM, NPMAX, NPMIN, NPTIMP, NP, NPIMP, NVVEC, NU, NV, NW.

TMAX0.1

CFLC0.025

CFLV0.025

DTPLOT0.005

PLANE WAVE (default) is used on all boundaries.

The default settings are used.

The pressure history for monitor points 6, 7 and 10 (front of the structure closest to the blast) are presented below. This region experiences the maximum impact of the explosion with overpressures of over 25 bar.

Figure 7.33: Pressure history for monitor points 6, 7

0                      1                      2                      3                      4                      5

TIME (ms)

Run:100000

Var: Pressure


and 10.


The plots below show the pressure history on the top and back of the same pressures are under 1 bar.

structure. Here the maximum


^<-ro^^①」nss①」d



0

Run: 100000 Var: Pressure


-0.05

5

2 o.

o 2 o.

5 0 5 0

1 1 o o 0.0.0.0.



^<~ro^^①」nss①」d



0

Run: 100000 Var: Pressure


0.10

0.05

0.00

-0.05

-0.10


-MP 3



20


40     60     80     100

TIME (ms)


Figure 7.34: Pressure history for the top (left) and back (right) of structure 1.

Next, the pressure history on the sides of the same structure and for the monitor points located opposite to the structures are displayed. On the sides, the maximum pressure is under 1 bar, while monitor point 20 records a maximum overpressure of over 12 bar.

(6(uq)①」nss①」j



0


-0.2

.86 o.o.

4 2 0 o.o.o.

5

20

10        15

TIME (ms)

0       1

Run:100000

Var: Pressure


Run:100000

Var: Pressure


Figure 7.35: Pressure history for the sides of structure 1 (left) and opposite the structures (right).

The results for monitor points on the structure behind the first box are shown below. The overpressures for this structure are considerably lower than for the first box, with a maximum level of just over 0.25 bar. This is consistent with the fact that this structure does not experience the full impact of the blast. Also the overpressures for locations on the side of the structures are shown below.


Figure 7.36: Pressure history for structure 2 (left) and on the side of the structures (right).


Finally, the pressure contours between 0 and 1 bar at 5 ms are presented, showing the shape and size of the blast wave.

Run100000

Var Pressure_3D (volume) Time: 0.005 —(1)



Figure 7.37: Illustration of the blast wave after 5 ms.

As noted in the section on the application areas of FLACS-CFD, it is important to be aware of assumptions and limitations that are inherent to the models used for simulating flow phenomena. This section identifies such characteristics for the FLACS-CFD software.

It is important to include sufficiently fine details in the geometry model, for a typical industrial installation or oil/gas rig on a scale of 100m typically down to about 1-inch piping and even smaller dimensions for pipe racks, cable trays, etc. For modern process plants, it is often possible to import the geometry model from existing computer aided design (CAD) models. However, for older facilities, or during the design phase of new ones, safety engineers must seek other solutions.

There are several known issues and inherent limitations associated with the representation of complex geometries in FLACS-CFD, including:

There are several known issues and limitations associated with the simulation of release and dispersion scenarios in FLACS-CFD and FLACS-Dispersion:

Jet utility program,

Flash utility program.

(i.e., non-isentropic) expansion (over-expanded jet) without air entrainment; or expansion over a normal shock to ambient pressure. These assumptions are not appropriate for very high reservoir pressures and/or temperatures, or for particle- or droplet-laden flows.

There are several inherent limitations and important guidelines associated with the simulation of gas explosion scenarios in FLACS-CFD and FLACS-GasEx, including:

For mixed fuels especially at elevated pressures and/or temperatures.

For ”initial pressures significantly below 1 atmosphere”.

For further guidance and possible workarounds contact FLACS-CFD support.

FLACS-Hydrogen is a CFD-code for simulating dispersion and explosion scenarios with hydrogen gas in complex geometries. All functionality of FLACS-Hydrogen can be found in the full FLACS-CFD package. Important changes regarding the hydrogen combustion properties:

These changes result from extensive validation including the following experiments:

Based on these simulation results, the performance of FLACS-CFD simulating hydrogen is considered comparable to what is generally seen when simulating other gases.

The dynamic viscosity for hydrogen in FLACS-CFD with default settings may be somewhat too high. This will only be important in situations with absolutely no turbulence, e.g., in closed vessels with no ventilation and weak temperature gradients. Upon discovery of this issue it was decided not to change the default values; instead it has been made possible to define the constant for dynamic viscosity manually in a setup-file or using the KEYS field in the scenario file. The default constant for dynamic laminar viscosity in FLACS-CFD is 2.0e-5, a more appropriate value is 0.6e-5. If needed, it may be changed using a setup file, as shown below:

VERSION 1.1

$SETUP

KEYS="AMUL=Y:0.6e-5"

$END

A sensitivity study has shown that simulation results usually are relatively insensitive to changing AMUL. Regarding time stepping when simulating hydrogen, the standard guidelines should be applied, i.e. CLFC=5 and CFLV=0.5

FLACS includes a model for predicting overpressures after transition to detonation. For hydrogen this transition is automatically triggered based on the DPDX criterion. For other gasses, where detonation is less likely, it must be enabled manually by the user. The following should be noted:

There are several inherent limitations and important guidelines associated with the simulation of jet and pool fires in FLACS-Fire, including:

There are several known issues and inherent limitations associated with the simulation of dust explosion scenarios with FLACS-DustEx, including:

In addition to the above limitations for FLACS-CFD, the following further limitations should be taken into account when simulating blast wave propagation with FLACS-Blast:

The models included in FLACS-Blast work well for far-field blast propagation; near-field results and internal explosions may be unreliable.

Regarding far-field blast simulations with FLACS-CFD, Hansen et al. (2010) and Hansen & Johnson (2014) suggested a method to improve the preservation of the form of the pressure wave by a suitably timed reduction of the time step. Typically this will require a simulation with the normal time step first, and the total simulation time will be increased by a factor 4-5. Gexcon has compared the results using the proposed method with the multi-energy curves from TNO; while the pressure predictions in the far-field tend to be improved, the form of the curves is still quite different. When applying the method, one has to be careful not to reduce the time step before the pressure wave has left the flame front, as this can affect the combustion rate and change the source pressure.

Some inherent inaccuracy will be introduced by the representation of imported terrain as blocks on the Cartesian grid. Primarily this will contribute to the generation of additional artificial turbulence near the ground. In addition, the stepped representation of the ground surface can affect the dispersion of vertically stratified flows resulting from the release of dense gases.

For gas dispersion the artificial turbulence will increase mixing and diffusion near the ground and thus reduce calculated dispersion results, especially in the far field (e.g., 100 m-200 m from the release). This effect is expected to be strongest for dense plume/jet dispersion (where negative buoyancy forces dominate) with the gas cloud flowing close to the terrain level. In addition, in vertically stratified flows, the stepped representation of the terrain surface may enhance the separation of cloud layers with different densities leading to an artificial confinement of denser layers. Fewer issues are expected for passive plume/jet dispersion (where the release momentum and ambient turbulence dominate the dispersion) or for positively buoyant plume/jet dispersion. It is therefore recommended to use a terrain to represent to the ground surface for passive dispersion scenarios, but, until further validation is done, it is recommended that terrains are used with caution when simulating the active dispersion of dense gases, and a grid sensitivity study is generally advisable. To determine if a plume of dense gas is passive or active, typically one of the variations of the Richardson number can be used. For full scale dense gas dispersion where the source momentum is unimportant (e.g., pool evaporation), the following criterion for passive plumes can be used (Britter, 1988):

Uref— > 6 g0q0              6,

(7.2)


D

where, Uref [m/s] is the wind speed at 10 m height, go = g (pgas - Pair)/pair [m/s2] is the reduced gravity, and D [m] is the characteristic horizontal dimension of the leak or pool.

Note that this criterion is relatively strict, so most pool dispersion scenarios will be classified as active.

For dense jets, mixing is triggered by the release momentum instead of the ambient wind. In these cases, the densimetric Froude number replaces the Richardson number in the definition of passive conditions:

Uleak

(7.3)


VgVD   ,

where, Uieak [m/s] is the leak velocity, go = g (Pgas Pair)/Pair [m/s2] is the reduced gravity, and D [m] is the diameter of the jet.

It is recommended to use a relatively fine vertical grid resolution Az (e.g. 20 cm - 50 cm) near the imported terrain and a corresponding horizontal resolution Ax Az/sx and Ay Az/sy based on the local slopes sx and sy , respectively, in the x and y directions. For further recommendations regarding grid resolution, see grid bestpractice. In line with the existing dense gas dispersion recommendation, it is also recommended to model dispersion over terrain with a maximum slope of 10° only.

For explosion and fire simulations no significant issues are expected for the terrain functionality. However, for deflagrations where the gas cloud is on top of a terrain, a slight increase in explosion overpressures is expected due to the additional artificial turbulence over the terrain, but this effect is expected to be very modest. For fire simulations, the box approximation of the terrain may influence the radiation pattern and may result in local over- or under-estimation.

FLACS-CFD v22.2 User’s Manual

GEXCON